# coupling temperature between two solids

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Display Modes
January 13, 2011, 16:54
coupling temperature between two solids
#1
Senior Member

Mirko Vukovic
Join Date: Mar 2009
Posts: 159
Rep Power: 8
Hi,

I am trying to figure out how to solve a temperature conduction problem between two solids using chtMultiRegionFoam. There are no fluids in this problem.

My problem is that I don't know how to couple the temperature across the solid boundaries. I have tried using the solidWallMixedTemperatureCoupled, but that does not work

Code:
```        air_to_plate
{
type           solidWallMixedTemperatureCoupled;
neighbourFieldName T;
K          K;
value          293.15;
}```
(disregard the meaning of the `air' label - that is from a solid-fluid version of the problem when air was a fluid. Now I am treating it as solid).

As the problem in the solver that I am using or in the boundary condition?

Thanks,

Mirko

PS - I am attaching the problem files for a simple 2D problem.
Attached Files
 two-region-heat-conduction.tar.gz (6.1 KB, 10 views)

 January 14, 2011, 05:25 coupledMatrix #2 New Member   Maria Join Date: Apr 2009 Posts: 12 Rep Power: 8 Did you try using the "coupledMatrix" instead? (See conjugateHeatFoam) Marķa

January 14, 2011, 10:55
#3
Senior Member

maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 12
Hi Mirko,
Quote:
 Originally Posted by mirko Hi, I am trying to figure out how to solve a temperature conduction problem between two solids using chtMultiRegionFoam. There are no fluids in this problem.
I run a case like that as well, and the solution is as expected (at least in the temperature distribution). What I have is:
constant/solid1/polymesh/boundary file:
Code:
```    solid1_to_solid2
{
type            directMappedWall;
nFaces          10;
startFace       390;
sampleMode      nearestPatchFace;
sampleRegion    solid2;
samplePatch     solid2_to_solid1;
offset          (0 0 0);
}```
and 0/solid1/T file:
Code:
```    solid1_to_solid2
{
type            solidWallMixedTemperatureCoupled;
value           uniform 300;
neighbourFieldName T;
K               K;
}```
That's it! Hope it helps.
mad

January 14, 2011, 15:10
#4
Senior Member

Mirko Vukovic
Join Date: Mar 2009
Posts: 159
Rep Power: 8
Quote:
 Originally Posted by maddalena Hi Mirko, I run a case like that as well, and the solution is as expected (at least in the temperature distribution). What I have is: constant/solid1/polymesh/boundary file: Code: ``` solid1_to_solid2 { type directMappedWall; nFaces 10; startFace 390; sampleMode nearestPatchFace; sampleRegion solid2; samplePatch solid2_to_solid1; offset (0 0 0); }``` and 0/solid1/T file: Code: ``` solid1_to_solid2 { type solidWallMixedTemperatureCoupled; value uniform 300; neighbourFieldName T; K K; }``` That's it! Hope it helps. mad
Thank you!

Yep, it helped me track down an incorrect entry in the changeDictionary/dictionaryReplacement/boundary/X_to_Y. I had incorrectly set the sampleRegion as X instead of Y.

I also used the coupling boundary condition compressible::turbulentTemperatureCoupledBaffle (I don't have a clue why that name. Looking at it's .H file the coupling condition looks very general).

Mirko

 January 17, 2011, 03:28 #5 Senior Member     maddalena Join Date: Mar 2009 Posts: 436 Rep Power: 12 Hi Mirko, could you post the temperature change in time of some points of your domain and compare them with theoretical time variation? I have some doubts on results I have obtained so far... Thank you mad

 January 17, 2011, 10:48 link #6 Senior Member     maddalena Join Date: Mar 2009 Posts: 436 Rep Power: 12 posted something on the subject here: http://www.cfd-online.com/Forums/ope...tml#post290772 mad

January 17, 2011, 12:00
#7
Senior Member

Mirko Vukovic
Join Date: Mar 2009
Posts: 159
Rep Power: 8
Quote:
 Originally Posted by maddalena Hi Mirko, could you post the temperature change in time of some points of your domain and compare them with theoretical time variation? I have some doubts on results I have obtained so far... Thank you mad
I want to cleanup my setup & generate some benchmark cases. I will then post my setup and results.

Mirko

January 19, 2011, 18:58
#8
Senior Member

Mirko Vukovic
Join Date: Mar 2009
Posts: 159
Rep Power: 8
Quote:
 Originally Posted by maddalena Hi Mirko, could you post the temperature change in time of some points of your domain and compare them with theoretical time variation? I have some doubts on results I have obtained so far... Thank you mad
Hi Maddalena,

(got busy with paperwork)

Unfortunately, I managed to break my two-region problem and loose the temperature connectivity across the interface.

FWIW I am attaching two archives:
1. The broken two region problem that illustrates my predicament
2. A simple 1D thermal conduction problem that I wanted to use for benchmarking of the above model. This is a very unphysical one: temperatures between 0 & 1. This simple model is working.
Thanks,

Mirko
Attached Files
 two-region-heat-conduction.tar.gz (4.2 KB, 9 views) 3146--single-region-1D-heat-conduction-benchmark.tar.gz (3.4 KB, 6 views)

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Mihail CFX 7 September 7, 2014 06:27 tensun Fluent UDF and Scheme Programming 0 November 14, 2010 06:30 sheintz STAR-CCM+ 3 September 30, 2010 13:56 shahpar73 CFX 2 August 20, 2009 18:51 Brett Towler CFX 1 September 20, 2000 20:09

All times are GMT -4. The time now is 00:33.

 Contact Us - CFD Online - Top